Complete DFM Guide for CNC Machining

Design for Manufacturability best practices to reduce cost, improve quality, and shorten lead time for CNC machined parts. Used by 10,000+ engineers worldwide.

1. Wall Thickness Recommendations

Minimum wall thickness depends on the material, part size, and wall height. Thinner walls vibrate during machining, causing poor surface finish and dimensional inaccuracy. Use the table below as a starting point.

Material	Minimum	Recommended	Notes
Aluminum 6061/7075	0.5 mm	1.0–1.5 mm	Below 0.8 mm risk vibration and deflection during machining
Stainless Steel 304/316	0.5 mm	1.0–2.0 mm	Work hardening increases difficulty on thin walls
Carbon Steel 1018/4140	0.8 mm	1.5–2.0 mm	Heat treatment may warp thin sections
Titanium Grade 5	0.5 mm	1.0–1.5 mm	Spring-back requires extra support. Slow cutting speeds.
Brass C360	0.5 mm	0.8–1.0 mm	Excellent machinability allows thinner walls than steel
PEEK / Delrin	1.0 mm	1.5–2.0 mm	Plastics deform under clamping pressure. Larger radii needed.
Inconel 718	0.8 mm	1.5–2.5 mm	Very difficult to machine. Tool pressure can distort thin walls.

2. Internal Corner Radius

CNC end mills are round, so every internal corner will have a radius equal to the tool radius. Designing for this is one of the single biggest cost-saving DFM optimizations.

Key Rules:

1Minimum radius = 1/3 of pocket depth. A 9 mm deep pocket should have at least R3 mm internal corners.
2Use consistent radii. If your part has 5 pockets, use the same corner radius for all of them. This minimizes tool changes.
3Avoid R0 (sharp) internal corners. These require EDM, adding $200–$1000+ per feature. If a mating part needs a sharp corner, add a relief groove on one part instead.
4Standard tool sizes: R1.5, R2, R3, R4, R5, R6 mm. Design to these values for fastest delivery.

3. Hole Depth-to-Diameter Ratios

Deeper holes require longer drill bits that are more prone to deflection and breakage. Design within standard ratios to minimize cost and improve accuracy.

Hole Type	Max Depth:Dia	Example	Notes
Standard drill	4:1	6 mm dia × 24 mm deep	Most cost-effective. Standard tooling available.
Deep hole drill	10:1	6 mm dia × 60 mm deep	Requires peck drilling. Higher cost, slower feed rates.
Gun drill	20:1+	6 mm dia × 120 mm+ deep	Specialized tooling. Longest lead time and highest cost.
Reamed hole	4:1	6H7 × 24 mm deep	Tight tolerance bore. Must be drilled first, then reamed.
Tapped hole	3:1	M6 × 18 mm deep	Thread engagement = 2× diameter minimum for steel.

4. Thread Design Guidelines

Proper thread design prevents tap breakage, ensures reliable fastening, and keeps cost down.

Guideline	Recommendation	Reason
Minimum thread engagement	3 full threads (2× diameter in steel, 2.5× in aluminum)	Below 3 threads, joint fails at the thread rather than the bolt
Preferred thread sizes	M3, M4, M5, M6, M8, M10 (or #4-40, #6-32, 1/4-20, 3/8-16)	Standard sizes = standard taps = lower cost and faster delivery
Thread relief	Add 0.5–1.0 mm relief groove at thread runout	Allows full thread engagement without interference at bottom
Blind threaded holes	Add 2–3 pitch lengths clearance below last thread	Tap needs runout space; avoids bottoming and tap breakage
Custom threads	Avoid if possible. Use standard metric or unified threads.	Custom thread mills cost 5–10× more than standard taps
Thread inserts (Helicoil)	Use in aluminum and plastics for M5+ threads	Prevents thread stripping in soft materials under repeated use

5. Undercut Considerations

Undercuts are features that cannot be reached by a standard end mill approaching from above. They require special tooling (T-slot cutters, lollipop cutters, or dovetail cutters) or additional setups.

Do:

Use standard T-slot or dovetail dimensions when possible
Design undercuts accessible from at least one open side
Specify undercut width, depth, and radius clearly on drawings
Consider if the undercut can be replaced by a through-pocket

Don't:

Design enclosed undercuts that need multi-axis EDM
Require undercuts deeper than 2x the opening width
Place undercuts in deep pockets where tool reach is limited
Assume undercuts are “free” — each one adds setup time

6. Tolerance Selection: When It Matters vs. Wasted Money

Tolerancing is the biggest hidden cost driver in CNC machining. Every dimension that requires inspection beyond “within general tolerance” adds time and cost.

Worth Tight Tolerance:

✓Bearing bores and shaft fits (H7/g6)
✓O-ring groove dimensions
✓Dowel pin holes for alignment
✓Mating surfaces between assembly parts
✓Lens or optical element mounting

Not Worth Tight Tolerance:

✗Overall part dimensions (length, width)
✗Clearance holes for bolts
✗Non-mating edges and surfaces
✗Decorative features and chamfers
✗Internal pocket dimensions (non-critical)

See our Tolerance Chart for achievable tolerances by process.

7. Surface Finish vs. Cost Tradeoff

Each halving of the Ra value roughly doubles the finishing cost. Specify the roughest acceptable finish to save money.

Ra 3.2 μm

As-machined (standard)

Ra 1.6 μm

1.2x

Fine machined

Ra 0.8 μm

1.5x

Precision finish

Ra 0.4 μm

Ground / polished

Ra 0.1 μm

Mirror finish

See our Surface Finish Chart for detailed Ra values and process methods.

8. File Format Recommendations

PREFERRED

STEP (.stp / .step)

Universal 3D format. Preserves exact geometry. Supported by all CAM software. Fastest quoting and programming.

ACCEPTED

Native CAD Files

SolidWorks (.sldprt), Inventor (.ipt), Creo/Pro-E (.prt), Fusion 360 (.f3d). Preserves design intent and feature tree.

ACCEPTED

IGES (.igs / .iges)

Older universal format. Surface-based (not solid). May have translation issues with complex surfaces. Use STEP when possible.

SUPPLEMENT ONLY

2D Drawing (PDF / DXF)

Essential for tolerances, surface finish, and special notes. Always pair with a 3D model. Never submit 2D only for complex parts.

9. Common DFM Mistakes Checklist

Sharp internal corners

Fix: Add radius ≥ 1/3 of pocket depth. Minimum R0.5 mm for most tools.

Cost impact: Requires EDM or special tooling, adding 2–3× cost.

Unnecessary tight tolerances

Fix: Tolerance only mating/functional surfaces. Use general tolerance block.

Cost impact: Each over-toleranced feature adds 15–30% inspection time.

Deep narrow pockets

Fix: Keep depth-to-width ratio below 4:1. Add corner radii.

Cost impact: Requires long, thin tools that deflect and break easily.

Thin walls without support

Fix: Min wall 1.0 mm for metals, 1.5 mm for plastics. Add ribs if needed.

Cost impact: Vibration causes chatter, poor finish, and dimensional errors.

Text engraving too small

Fix: Minimum font height 5 mm, line width 0.5 mm for milling.

Cost impact: Small text requires micro-tools with very slow feed rates.

Undercuts without clearance

Fix: Design for standard T-slot or dovetail cutters. Specify undercut dimensions.

Cost impact: Non-standard undercuts need custom tooling ($500–$2000).

Missing 3D model

Fix: Always provide STEP file alongside 2D drawing.

Cost impact: Delays quoting by 1–2 days. Increases programming errors.

Over-specifying surface finish

Fix: Use as-machined (Ra 3.2) where appearance is not critical.

Cost impact: Mirror finish costs 2–3× standard. Specify only where needed.

DFM Deep Dive Articles

Wall Thickness Guidelines for CNC Parts

Read article

Internal Corner Radius Design Rules

Read article

Hole Design Best Practices

Read article

Thread Design for CNC Machining

Read article

Undercut Design Considerations

Read article

Tolerance Selection Guide

Read article

Surface Finish vs Cost Tradeoff

Read article

File Format Best Practices

Read article

Common DFM Mistakes to Avoid

Read article

DFM Checklist for Engineers

Read article

Frequently Asked Questions

What is DFM (Design for Manufacturability)?

DFM is the practice of designing parts to be easy and cost-effective to manufacture. For CNC machining, DFM involves optimizing wall thickness, corner radii, hole depths, tolerances, and surface finishes to reduce machining time, tooling cost, and scrap rate while maintaining part function.

Why are internal sharp corners a problem in CNC machining?

CNC cutting tools are round, so they naturally leave a radius in internal corners equal to the tool radius. Achieving sharp internal corners requires additional operations like EDM (Electrical Discharge Machining), which can increase cost by 2-3x. Adding a radius of at least 1/3 the pocket depth eliminates this issue.

What is the minimum wall thickness for CNC machined parts?

Minimum wall thickness depends on material: 0.5 mm for aluminum and brass, 0.8 mm for steel and titanium, and 1.0 mm for plastics. However, recommended minimums are 1.0-1.5 mm for metals and 1.5-2.0 mm for plastics to avoid vibration and deformation during machining.

What file format should I use for CNC machining quotes?

STEP (.stp/.step) is the preferred format as it preserves exact geometry and is universally supported by CAM software. Also accepted: IGES, SolidWorks (.sldprt), Inventor (.ipt), Creo (.prt). Always include a 2D PDF drawing with tolerances and surface finish callouts alongside the 3D model.

How much does DFM optimization reduce part cost?

Proper DFM optimization typically reduces CNC machining cost by 20-50%. The biggest savings come from: relaxing non-critical tolerances (10-20% savings), adding internal corner radii (15-30%), optimizing wall thickness to avoid secondary operations (10-15%), and using standard hole sizes and thread specs (5-10%).

What is the maximum depth-to-width ratio for CNC pockets?

The recommended maximum depth-to-width ratio for CNC milled pockets is 4:1. Beyond this, long tools deflect under cutting forces, causing poor surface finish and dimensional inaccuracy. For ratios up to 6:1, use reduced feed rates. Beyond 6:1, consider EDM or redesigning the feature.

Do you provide free DFM review?

Yes, we provide free DFM feedback on every quote request. Our engineering team reviews your design and suggests modifications to reduce cost, improve quality, and shorten lead time. Upload your 3D model and we will return a detailed DFM report within 24 hours.

Should I design for 3-axis or 5-axis machining?

Design for 3-axis when possible, as it is more widely available and cost-effective. If your part has features on multiple faces, undercuts, or complex contours that would require more than 3 setups on a 3-axis machine, designing for 5-axis can actually reduce total cost despite higher hourly rates.

How do I reduce CNC machining cost without changing my design?

Without design changes: 1) Increase order quantity for volume discounts, 2) Choose a more machinable material (e.g., 6061 vs 7075), 3) Relax non-critical tolerances, 4) Accept as-machined finish where possible, 5) Allow longer lead times to avoid rush fees, 6) Batch similar parts to share setup costs.

What is the difference between general and critical tolerances?

General tolerances (specified in the title block, e.g., ±0.1 mm) apply to all non-specified dimensions. Critical tolerances are tighter values called out on specific features that must mate with other parts or meet functional requirements. Only 10-20% of dimensions typically need critical tolerances.

Upload Your Design for Free DFM Review

Our engineering team will review your design and provide actionable DFM feedback within 24 hours — completely free, no obligation.

Get Free DFM Review